Change part reference in a drawing

I create many parts that are very similar but don't want to completely redraw my part and then the drawing. I also don't want to have a part with different configurations as these parts are used in different products and I don't want the same part number.

I used to use Inventor and this was extremely easy and I can't get the same result in SW. (2012 standard, SP2).

I create a part and the related drawing with all the notes, blocks, etc. that I want. Lets say it is part ABC01 and drawing ABC01.

Then I do a Save-As (or Save Copy As) on both the part and the drawing with a new part number. Lets say they are part ABC02 and drawing ABC02.

Then close all drawings and parts.

If I was to just open the new drawing (ABC02) at this point it would reference the original part (ABC01) since this was the original referenced part.

I don't want it to reference ABC01, so before opening the new drawing I change the name of the original part so it is not recognized. Lets say to ABC01x.

Now I open the drawing ABC02 and it will not find the referenced part and ask me to find it.

I will then select ABC02 part in the open window (again this is the operation in Inventor - but SW works similar up to this point).

My drawing will open with the reference to part ABC02 and the parts and related drawings are now separated.

Then I just rename the ABC01x back to ABC01 and I have 2 parts (identical) and 2 drawings - one for each part.

Then I can make the changes to part ABC02 with the ABC02 drawing following that part and not ABC01.

When I try this in SW it seems that everything works except all I get is view outlines were all my views were with lines (forming an X in the view) from the corners.

When I got to the file menu and select find references it shows the drawing and the part both in the list with the new names.

If I select a view and then select the Open part it will open the new part file with no problems.

It will even display annotations in some of the views if I go to those views and select to import the annotations.

I am not sure why the views are being hidden by going through the steps that you have. I tried the same thing on SolidWorks 2012 and I do not see the problem. I only get that type of problem if I choose NOT to browse for the replacement part when it doesn't find it.

However, I wanted to let you know there is a MUCH easier way to do what you are trying to do.

With the original drawing open, when you go to Save As (or Save As Copy), put in the new name of the drawing that you want (ABC02 for instance) click on the References button in the Save dialog and then put in the new name for the part (again, ABC02 for example). Then hit Save All. That should do the same exact thing that you are trying to do in much fewer steps.

I am not sure why the views are being hidden by going through the steps that you have. I tried the same thing on SolidWorks 2012 and I do not see the problem. I only get that type of problem if I choose NOT to browse for the replacement part when it doesn't find it.

However, I wanted to let you know there is a MUCH easier way to do what you are trying to do.

With the original drawing open, when you go to Save As (or Save As Copy), put in the new name of the drawing that you want (ABC02 for instance) click on the References button in the Save dialog and then put in the new name for the part (again, ABC02 for example). Then hit Save All. That should do the same exact thing that you are trying to do in much fewer steps.

Likewise to Jim's input, if you have already performed the "Save As Copy" for the drawing and part file but did not re-reference the new drawing to the new part, you can achieve this in the File>Open dialog. Select the new drawing in the list and click the References... button. The Edit Referenced File Locations dialog will open and show the original part and path. Update to the new part name.

Jim's is a more direct workflow. But this is a close second if your files already exist.

There is another way to do what you want. With the drawing open you can do a Pack and Go. In the Pack and Go dialog box there is a column where you can double-click on the file names and assign new names. (I'm at home now and don't have SW here to get the column name.)